Linear Static Analysis of a Simply-Supported Truss
|
|
- Eugenia Lynch
- 6 years ago
- Views:
Transcription
1 WORKSHOP PROBLEM 2 Linear Static Analysis of a Simply-Supported Truss Objectives: Define a set of material properties using the beam library. Perform a static analysis of a truss under 3 separate loading conditions. Review results. MSC/NASTRAN 101 Exercise Workbook 2-1
2 2-2 MSC/NASTRAN 101 Exercise Workbook
3 WORKSHOP 2 Simply-Supported Truss Model Description: Below is a finite element representation of the truss structure shown on page 2-1. The nodal coordinates provided are defined in the Global Cartesian Coordinate System (MSC/NASTRAN Basic system). The roof frame shown in the attached figure consists of eleven wood and steel members. The wood members, have uniform cross section properties and act only as tension and compression members. (See page 2-5 for location.) The steel members, are bars that are capable of withstanding tension, compression, shear, and loads in the plane of the frame. (See page 2-5 for location.) The section properties for the steel members are supplied as problem data. All the steel members are welded end to end, however, the wood members are pinned end to end. The frame is supported by pinned connections in the horizontal and vertical directions at Grid Point 1 and in the vertical direction at Grid Point 7. In addition, all Grid Points have fixed out of plane translations and have constrained out of plane rotations. Hint: DOF 345 for grid 1 thru 7 can be constrained by using the permanent single point constraint option in the GRID entry. Grid Coordinates and Element Connectivities [288,144,0] 4 1 [0,0,0] [144,72,0] [432,72,0] [192,0,0] [384,0,0] 7 [576,0,0] Y Z X MSC/NASTRAN 101 Exercise Workbook 2-3
4 Loads and Boundary Conditions Snow Drift 100 pounds/inch maximum Ambient Temperature 32 deg. F Ambient Temperature 100 deg. F Y Concentrated Load 2000 pounds Z X Interior Temperature applied 36 inches from Grid Point 3 60 deg. F. Subcase One will be only the gravity load due to the weight of both the wood and steel members. Subcase Two will be the snow drift load and the concentrated load. The snow drift load is in the vertical direction and is given as a varying running load. The load increases linearly with distance along the beam, from 0 at Grid Point 4 to 100 lbs/in. at Grid Point 1. Subcase Three will be the temperature load which is calculated as the temperature averages and applied at the joints. The joint temperatures are supplied as problem data. The stress-free reference temperature is 72.0 degrees F. 2-4 MSC/NASTRAN 101 Exercise Workbook
5 WORKSHOP 2 Simply-Supported Truss Table 2.1 Table 2.2 Description of Element Properties material element type and cross setion Top members, elements 1, 2, Steel Beam, Cross Section B 3, and 4 Bottom members 9, 10 and 11 Steel Beam, Cross Section A Interior members 5, 6, 7, 8 Southen Pine Rod, Area = 5.2 in2 Material Properties Matieral Steel Southern Pine Elastic Modulus 2.90E 7 psi 1.76E 6 psi Poisson s Ratio 0.32 Mass Density 7.349E -4 lbm/in E -5 lbm/in4 Coefficient of Thermal Expansion 6.78E-6 in/deg. F 3.00e-6 in/deg. F Reference Temperature 72 deg. F 72 deg. F Allowable tension stress psi 1900 psi Allowable compression stress psi 1900 psi Allowable shear stress psi Gravitational Acceleration in/sec in/sec2 MSC/NASTRAN 101 Exercise Workbook 2-5
6 Table 2.3 Beam Dimensions Cross Section A Cross Section B H 8.0 in. 6.0 in. W1 3.0 in. 3.0 in. W2 3.0 in. 3.0 in. t 0.5 in. 0.5 in. t1 0.5 in. 0.5 in. t2 0.5 in. 0.5 in. Table 2.4 Temperature Distribution Joint Values 1 45 deg. F deg. F deg. F deg. F deg. F deg. F deg. F. 2-6 MSC/NASTRAN 101 Exercise Workbook
7 WORKSHOP 2 Simply-Supported Truss Suggested Exercise Steps: Generate a finite element representation of the truss structure using (GRID), (CROD), and (CBAR) elements. (Hint: Remember to use permanent constraints for DOF 345.) Define material (MAT1) and element (PROD) and (PBARL) properties. simply-supported boundary constraints (SPC1), inertial loads (GRAV), a temperature load (TEMP), and a distributed load (PLOAD1). Use the load and boundary condition sets to define loadcases (SUBCASE). Prepare the model for a linear static analysis (SOL 101). Submit it for a linear static analysis. Review results. MSC/NASTRAN 101 Exercise Workbook 2-7
8 ID SEMINAR,PROB2 CEND BEGIN BULK 2-8 MSC/NASTRAN 101 Exercise Workbook
9 WORKSHOP 2 Simply-Supported Truss MSC/NASTRAN 101 Exercise Workbook 2-9
10 ENDDATA 2-10 MSC/NASTRAN 101 Exercise Workbook
11 WORKSHOP 2 Simply-Supported Truss Exercise Procedure: 1. Users who are not utilitizing MSC/PATRAN for generating an input file should proceed to Step 20, otherwise, continue with step Create a new database called prob2.db. File/New... New Database Name: prob2 In the New Model Preferences form set the following: Tolerance: Analysis Code: Analysis Type: Default MSC/NASTRAN Structural 3. Select a preset view by selecting the Front View icon on the toolbar. Front View 4. Activate the entity labels by selecting the Show Labels icon on the toolbar. Show Labels 5. Create the nodes by manually defining their respective coordinates: Finite Elements Action: Create Object: Node Method: Edit Associate with Geometry MSC/NASTRAN 101 Exercise Workbook 2-11
12 Node Location List: [0, 0, 0] Repeat the previous operation to create the remaining nodes. Refer to the figure on page 2-3 for the nodal coordinates. Node Location List: [144, 72, 0] Node Location List: [192, 0, 0] Node Location List: [288, 144, 0] Node Location List: [384, 0, 0] Node Location List: [432, 72, 0] Node Location List: [576, 0, 0] Next, manually define the truss segment connectivites with BAR2 elements using our newly created nodes. Again, refer to page 2-3 for connectivity information. Finite Elements Action: Create Object: Element Method: Edit Shape: Topology: Bar Bar MSC/NASTRAN 101 Exercise Workbook
13 WORKSHOP 2 Simply-Supported Truss Node 1 = Node 1 Node 2 = Node 2 Repeatthepreviousoperationuntilallthetrusssegmentshavebeencreated. Node 1 = Node 2 Node 2 = Node 4 Node 1 = Node 4 Node 2 = Node 6 Node 1 = Node 6 Node 2 = Node 7 Node 1 = Node 2 Node 2 = Node 3 Node 1 = Node 3 Node 2 = Node 4 Node 1 = Node 4 Node 2 = Node 5 Node 1 = Node 5 Node 2 = Node 6 MSC/NASTRAN 101 Exercise Workbook 2-13
14 Node 1 = Node 1 Node 2 = Node 3 Node 1 = Node 3 Node 2 = Node 5 Node 1 = Node 5 Node 2 = Node 7 Figure Nodal and Element Locations Y Z X 6. Next, define a material using the specified modulus of elasticity and allowable stresses. Materials Action: Create Object: Isotropic 2-14 MSC/NASTRAN 101 Exercise Workbook
15 WORKSHOP 2 Simply-Supported Truss Method: Manual Input Material Name: Input Properties... southern_pine Constitutive Model: Linear Elastic Elastic Modulus = 1.76E6 Density = 5.435E-5 Thermal Expan. Coeff = 3.00E-6 Reference Temperature = 72.0 Constitutive Model: Failure Tension Stress Limit = Compression Stress Limit =??? (Enter material limit)??? (Enter material Limit) In the Current Constitutive Models data box, you will see Failure - [n/a,,,,] - [Active] and Linear Elastic - [,,,,] - [Active] appear. Click on Cancel to close the form. Cancel 7. Define another material for the model, steel. Materials Action: Create Object: Isotropic Method: Manual Input MSC/NASTRAN 101 Exercise Workbook 2-15
16 Material Name: Input Properties... steel Constitutive Model: Linear Elastic Elastic Modulus = 2.90E7 Poisson Ratio = 0.32 Density = 7.349E-4 Thermal Expan. Coeff = 6.78E-6 Reference Temperature = 72.0 Constitutive Model: Failure Tension Stress Limit = Compression Stress Limit = Shear Stress Limit =??? (Enter material limit)??? (Enter material Limit)??? (Enter material Limit) In the Current Constitutive Models data box, you will see Failure - [n/a,,,,] - [Active] and Linear Elastic - [,,,,] - [Active] appear. Click on Cancel to close the form. Cancel 8. Next, reference the material that was created in the previous step. Define the properties of the truss segments using the specified cross-sectional data. Properties Action: Create 2-16 MSC/NASTRAN 101 Exercise Workbook
17 WORKSHOP 2 Simply-Supported Truss Dimension: 1 D Type: Rod Property Set Name: Input Properties... Material Name: Area: rod m:southern_pine??? (Enter cross-sectional area) Select Members: Elm 5:8 Add 9. Enter the properties for the steel members using bar elements with the beam library. Properties Action: Create Dimension: 1 D Type: Beam Property Set Name: Input Properties... Material Name steel_member_a m:steel Bar Orientation <0, 1, 0> Associate Beam Section MSC/NASTRAN 101 Exercise Workbook 2-17
18 Click the beam library icon: Action: Create Type: Standard Shape New Section Name: section_a H 8 W1 3 W2 3 t 0.5 t1 0.5 t2 0.5 Select Members: Elm 9:11 Add 10. Repeat the procedure for the remaining sections of the truss. Properties Action: Create Dimension: 1 D Type: Beam Property Set Name: Input Properties... steel_member_b 2-18 MSC/NASTRAN 101 Exercise Workbook
19 WORKSHOP 2 Simply-Supported Truss Material Name m:steel Bar Orientation <0, 1, 0> Associate Beam Section Click the beam library icon: Action: Create Type: Standard Shape New Section Name: section_b H 6 W1 3 W2 3 t 0.5 t1 0.5 t2 0.5 Select Members: Elm 1:4 Add 11. Shrink the elements by 10% for clarity; this allows us to easily assess the element connectivities. Use the Display/Finite Elements... option. Display/Finite Elements... FEM Shrink: 0.10 MSC/NASTRAN 101 Exercise Workbook 2-19
20 Cancel 12. Create three nodal constraints and apply them to the analysis model. These boundary conditions represent the simply-supported ends of the truss, the fixed out of plane translations, and the contrained rotations.. 12a. The left-hand support is defined as follows: Loads/BCs Action: Create Object: Displacement Type: Nodal New Set Name: Input Data... pin Translations < T1 T2 T3 > <0, 0, > Select Application Region... Geometry Filter: FEM Select Nodes: Node 1 Add 12b.The right-hand support is located at the opposite end of the truss. Loads/BCs Action: Create Object: Displacement Type: Nodal New Set Name: roller Input Data... Translations < T1 T2 T3 > <, 0, > 2-20 MSC/NASTRAN 101 Exercise Workbook
21 WORKSHOP 2 Simply-Supported Truss Select Application Region... Geometry Filter: FEM Select Nodes: Node 7 Add 12c. The out of plane translations and out of plane rotations can be constrained as follows: Loads/BCs Action: Object: Type: Create Displacement Nodal New Set Name: out_of_plane Input Data... Translations < T1 T2 T3 > <,,0> Rotations < R1 R2 R3 > <0, 0, > Select Application Region... Geometry Filter: FEM Select Nodes: Node 1:7 Add MSC/NASTRAN 101 Exercise Workbook 2-21
22 Figure Displacement Constraints Y Z X 12d.Reset the display by selecting the Reset Graphics icon on the Top Menu Bar. Reset Graphics 13. Deactivate the entity labels by selecting the Hide Labels icon on the toolbar. Hide Labels 14. Create the gravity load.. Loads/BCs Action: Create Object: Inertial Load Type: Element Uniform New Set Name: gravity_load Input Data... Load/BC Set Scale Factor: Trans Accel < A1 A2 A3 > <0, -1, 0> 2-22 MSC/NASTRAN 101 Exercise Workbook
23 WORKSHOP 2 Simply-Supported Truss Since the gravity load acts uniformly on the body, the application region is automatically set as the entire model. 15. Next, define the temperature load using fields. Fields Action: Create Object: Spatial Method: FEM Field Name: Input Data... temp_profile Enter the data into the table as shown below. Entity Values 1 Node Node Node Node Node Node Node 7 80 Loads/BCs Action: Create Object: Temperature MSC/NASTRAN 101 Exercise Workbook 2-23
24 Type: Nodal New Set Name: Input Data... Spatial Fields: temperature_load temp_profile (Click on this to select.) Select Application Region... Geometry Filter: FEM Select Nodes: Node 1:7 Add Figure Temperature Loads Y Y Z Z X X 2-24 MSC/NASTRAN 101 Exercise Workbook
25 WORKSHOP 2 Simply-Supported Truss 15a. Reset the display by selecting the Reset Graphics icon on the Top Menu Bar. Reset Graphics 16. Create a load case that references the inertial load and the boundary conditions that have already been defined. Load Cases Action: Create Load Case Name: Load Case Type: gravity_load Static Assign/Prioritize Loads/BCs Select all the Load/BC sets in the Select Loads/BCs to Add to Spreadsheet box by clicking on all of them. Highlight Loads/BCs to Add to Spreadsheet Displ_out_of_plane Displ_pin Displ_roller Inert_gravity_load * REMINDER: Make sure that the LBC Scale Factor column shows the proper value for each entry. 17. Create a second load case that references the temperature load, and the boundary conditions that have already been defined. Load Cases Action: Create Load Case Name: Load Case Type: temperature_load Static MSC/NASTRAN 101 Exercise Workbook 2-25
26 Assign/Prioritize Loads/BCs Select all the Load/BC sets in the Select Loads/BCs to Add to Spreadsheet box by clicking on all of them. Highlight Loads/BCs to Add to Spreadsheet Displ_out_of_plane Displ_pin Displ_roller Tempe_temperature_load If the inertial gravity load is in the spreadsheet, it can be removed as follows: Click the inertial gravity load in the spreadsheet. Remove Selected Rows 17a. Close the form. 18. Now you are ready to generate an input file for analysis. Click on the Analysis radio button on the Top Menu Bar and complete the entries as shown here. Analysis Action: Analyze Object: Entire Model Method: Analysis Deck Job Name: Translation Parameters... OUTPUT2 Format: MSC/NASTRAN Version: prob2 Binary??? Set accordingly, here it is MSC/NASTRAN 101 Exercise Workbook
27 WORKSHOP 2 Simply-Supported Truss Solution Type... Solution Type: Solution Parameters... Database Run Automatic Constraints Data Deck Echo: Linear Static Sorted Subcase Select... Subcases For Solution Sequence: Subcases Selected: gravity_load temperature_load (Click on these to select.) Default (Click on this to deselect.) An MSC/NASTRAN input file called prob2.bdf will be generated. This process of translating your model into an input file is called the Forward Translation. The Forward Translation is complete when the Heartbeat turns green. MSC/NASTRAN 101 Exercise Workbook 2-27
28 19. Modify prob2a.bdf to include a third subcase for the snow-drift load. Open the file prob2.bdf with a text editor. The text below defines a third subcase. Enter this text on the line before BEGIN BULK. SUBCASE 3 $ Subcase name : snow_&_concentrated_load SUBTITLE=snow & concentrated load spc = 2 load = 5 disp = all spcforce = all force = all This text describes the snow drift load for the third subcase, entire this text on the line before ENDDATA, which is at the very end of the file. PLOAD1,5,1,FY,FRPR,0.0,-100.,1.0,-50. PLOAD1,5,2,FY,FRPR,0.0,-50.,1.0,0.0 PLOAD1,5,10,FY,LE,36., MSC/PATRAN Users should proceed to step MSC/NASTRAN 101 Exercise Workbook
29 WORKSHOP 2 Simply-Supported Truss Generating an input file for MSC/NASTRAN Users: MSC/NASTRAN users can generate an input file using the data from the Model Description section at the beginning of the exercise. The result should be similar to the output below. 20. MSC/NASTRAN Input File: prob2a.dat ID SEMINAR,PROB2 TIME 5 SOL 101 CEND TITLE = GARAGE ROOF FRAME SUBTITLE = WOOD AND STEEL MEMBERS SPC = 20 DISP = ALL FORCE = ALL STRESS = ALL SPCFORCE = ALL SUBCASE 1 LABEL = GRAVITY LOAD LOAD = 1 SUBCASE 2 LABEL = TEMPERATURE LOAD TEMP(LOAD) = 2 SUBCASE 3 LABEL = SNOW AND CONCENTRATED LOAD LOAD = 3 BEGIN BULK GRID,1,,0.0,0.0,0.0,,345 GRID,2,,144.0,72.0,0.0,,345 GRID,3,,192.0,0.0,0.0,,345 GRID,4,,288.0,144.0,0.0,,345 GRID,5,,384.0,0.0,0.0,,345 GRID,6,,432.0,72.0,0.0,,345 GRID,7,,576.0,0.0,0.0,,345 CBAR,1,200,1,2,0.,1.,0. CBAR,2,200,2,4,0.,1.,0. CBAR,3,200,4,6,0.,1.,0. CBAR,4,200,6,7,0.,1.,0. CBAR,9,300,1,3,0.,1.,0. CBAR,10,300,3,5,0.,1.,0. CBAR,11,300,5,7,0.,1.,0. CROD,5,100,2,3 CROD,6,100,3,4 CROD,7,100,4,5 CROD,8,100,5,6 PROD,100,10,5.2 PBARL I PBARL I MAT1,10,1.76+6,,, ,3.0-6,72.,1900.,1900. MAT1,20,2.9+7,,.32, ,6.78-6,72.,24000.,24000., GRAV,1,,386.4,0.0,-1.0,0.0 PLOAD1,3,1,FY,FRPR,0.0,-100.,1.0,-50. MSC/NASTRAN 101 Exercise Workbook 2-29
30 PLOAD1,3,2,FY,FRPR,0.0,-50.,1.0,0.0 PLOAD1,3,10,FY,LE,36., TEMP,2,1,45. TEMP,2,2,32. TEMP,2,3,60. TEMP,2,4,66. TEMP,2,5,60. TEMP,2,6,100. TEMP,2,7,80. SPC,20,1,12,0.0 SPC,20,7,2,0.0 ENDDATA 2-30 MSC/NASTRAN 101 Exercise Workbook
31 WORKSHOP 2 Simply-Supported Truss SUBMITTING THE INPUT FILE FOR MSC/NASTRAN and MSC/PATRAN USERS: 21. Submit the input file to MSC/NASTRAN for analysis. 21a. To submit the MSC/PATRAN.bdf file for analysis, find an available UNIX shell window. At the command prompt enter: nastran prob2.bdf scr=yes. Monitor the run using the UNIX ps command. 21b. To submit the MSC/NASTRAN.dat file for analysis, find an available UNIX shell window. At the command prompt enter: nastran prob2 scr=yes. Monitor the run using the UNIX ps command. 22. When the run is completed, edit the prob2.f06 file and search for the word FATAL. If no matches exist, search for the word WARNING. Determine whether existing WARNING messages indicate modeling errors. 22a. While still editing prob2.f06, search for the word: D I S P L A C E (spaces are necessary). What are the components of the displacement vector for GRID 3 and 5 (translation only)? Gravity Load Case Temperature Load Case Snow Drift Load Case Grid 3 Grid 3 Grid 3 Disp. X = Disp. X = Disp. X = Disp. Y = Disp. Y = Disp. Y = Disp. Z = Disp. Z = Disp. Z = Grid 5 Grid 5 Grid 5 Disp. X = Disp. X = Disp. X = Disp. Y = Disp. Y = Disp. Y = Disp. Z = Disp. Z = Disp. Z = MSC/NASTRAN 101 Exercise Workbook 2-31
32 Search for the word: S I N G L E (spaces are necessary). What are the components of the reaction force at GRID 1 and GRID 7? Gravity Load Case Temperature Load Case Snow Drift Load Case GRID 1 GRID 1 GRID 1 T1 = T1 = T1 = T2 = T2 = T2 = T3 = T3 = T3 = GRID 7 GRID 7 GRID 7 T1 = T1 = T1 = T2 = T2 = T2 = T3 = T3 = T3 = Search for the word: F O R C E D I S T (spaces are necessary). What is the axial force in the BAR elements (CBAR) for each element case? Gravity Load Case Temperature Load Case Snow Drift Load Case Element 4 Element 4 Element 4 PCT PCT PCT PCT PCT PCT Element 11 Element 11 Element 11 PCT PCT PCT PCT PCT PCT What is the axial force in CROD elements 7 and 8? Gravity Load Case Temperature Load Case Snow Drift Load Case Element 7 Element 7 Element 7 Element 8 Element 8 Element MSC/NASTRAN 101 Exercise Workbook
33 WORKSHOP 2 Simply-Supported Truss Search for the word: S T R E S S (spaces are necessary). What is the margin of safety for elements 6 and 11? Gravity Load Case Temperature Load Case Snow Drift Load Case Element 6 Element 6 Element 6 PCT PCT PCT PCT PCT PCT Element 11 Element 11 Element 11 PCT PCT PCT PCT PCT PCT What is the Axial Stress for all elements 6 and 11? Gravity Load Case Temperature Load Case Snow Drift Load Case Element 6 Element 6 Element 6 PCT PCT PCT PCT PCT PCT Element 11 Element 11 Element 11 PCT PCT PCT PCT PCT PCT MSC/NASTRAN 101 Exercise Workbook 2-33
34 Comparison of Results: 23. Compare the results obtained in the.f06 file with the results on the next page MSC/NASTRAN 101 Exercise Workbook
35 MSC/NASTRAN 101 Exercise Workbook 2-35 GRAVITY LOAD D I S P L A C E M E N T V E C T O R POINT ID. TYPE T1 T2 T3 R1 R2 R3 1 G E-04 2 G E E E-06 3 G E E E-05 4 G E E E-19 5 G E E E-05 6 G E E E-06 7 G E E-04 TEMPERATURE LOAD D I S P L A C E M E N T V E C T O R POINT ID. TYPE T1 T2 T3 R1 R2 R3 1 G E-04 2 G E E E-04 3 G E E E-04 4 G E E E-04 5 G E E E-05 6 G E E E-06 7 G E E-04 SNOW AND CONCENTRATED LOAD D I S P L A C E M E N T V E C T O R POINT ID. TYPE T1 T2 T3 R1 R2 R3 1 G E-03 2 G E E E-03 3 G E E E-05 4 G E E E-03 5 G E E E-03 6 G E E E-05 7 G E E-04 WORKSHOP 2 Simply-Supported Truss
36 2-36 MSC/NASTRAN 101 Exercise Workbook GRAVITY LOAD F O R C E S O F S I N G L E - P O I N T C O N S T R A I N T POINT ID. TYPE T1 T2 T3 R1 R2 R3 1 G E E G E TEMPERATURE LOAD F O R C E S O F S I N G L E - P O I N T C O N S T R A I N T POINT ID. TYPE T1 T2 T3 R1 R2 R3 1 G E E G E SNOW AND CONCENTRATED LOAD F O R C E S O F S I N G L E - P O I N T C O N S T R A I N T POINT ID. TYPE T1 T2 T3 R1 R2 R3 1 G E E G E
37 MSC/NASTRAN 101 Exercise Workbook 2-37 GRAVITY LOAD F O R C E D I S T R I B U T I O N I N B A R E L E M E N T S ( C B A R ) ELEMENT STATION BEND-MOMENT SHEAR FORCE AXIAL ID. (PCT) PLANE 1 PLANE 2 PLANE 1 PLANE 2 FORCE TORQUE E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E F O R C E S I N R O D E L E M E N T S ( C R O D ) ELEMENT AXIAL ELEMENT AXIAL ID. FORCE TORQUE ID. FORCE TORQUE E E E E WORKSHOP 2 Simply-Supported Truss
38 2-38 MSC/NASTRAN 101 Exercise Workbook TEMPERATURE LOAD F O R C E D I S T R I B U T I O N I N B A R E L E M E N T S ( C B A R ) ELEMENT STATION BEND-MOMENT SHEAR FORCE AXIAL ID. (PCT) PLANE 1 PLANE 2 PLANE 1 PLANE 2 FORCE TORQUE E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E F O R C E S I N R O D E L E M E N T S ( C R O D ) ELEMENT AXIAL ELEMENT AXIAL ID. FORCE TORQUE ID. FORCE TORQUE E E E E
39 MSC/NASTRAN 101 Exercise Workbook 2-39 SNOW AND CONCENTRATED LOAD F O R C E D I S T R I B U T I O N I N B A R E L E M E N T S ( C B A R ) ELEMENT STATION BEND-MOMENT SHEAR FORCE AXIAL ID. (PCT) PLANE 1 PLANE 2 PLANE 1 PLANE 2 FORCE TORQUE E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E F O R C E S I N R O D E L E M E N T S ( C R O D ) ELEMENT AXIAL ELEMENT AXIAL ID. FORCE TORQUE ID. FORCE TORQUE E E E E WORKSHOP 2 Simply-Supported Truss
40 2-40 MSC/NASTRAN 101 Exercise Workbook GRAVITY LOAD S T R E S S D I S T R I B U T I O N I N B A R E L E M E N T S ( C B A R ) ELEMENT STATION SXC SXD SXE SXF AXIAL S-MAX S-MIN M.S.-T ID. (PCT) M.S.-C E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E+02 S T R E S S E S I N R O D E L E M E N T S ( C R O D ) ELEMENT AXIAL SAFETY TORSIONAL SAFETY ELEMENT AXIAL SAFETY TORSIONAL SAFETY ID. STRESS MARGIN STRESS MARGIN ID. STRESS MARGIN STRESS MARGIN E E E E E E E E
41 TEMPERATURE LOAD MSC/NASTRAN 101 Exercise Workbook 2-41 S T R E S S D I S T R I B U T I O N I N B A R E L E M E N T S ( C B A R ) ELEMENT STATION SXC SXD SXE SXF AXIAL S-MAX S-MIN M.S.-T ID. (PCT) M.S.-C E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E+01 S T R E S S E S I N R O D E L E M E N T S ( C R O D ) ELEMENT AXIAL SAFETY TORSIONAL SAFETY ELEMENT AXIAL SAFETY TORSIONAL SAFETY ID. STRESS MARGIN STRESS MARGIN ID. STRESS MARGIN STRESS MARGIN E E E E E E E E WORKSHOP 2 Simply-Supported Truss
42 2-42 MSC/NASTRAN 101 Exercise Workbook SNOW AND CONCENTRATED LOAD S T R E S S D I S T R I B U T I O N I N B A R E L E M E N T S ( C B A R ) ELEMENT STATION SXC SXD SXE SXF AXIAL S-MAX S-MIN M.S.-T ID. (PCT) M.S.-C E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E+01 S T R E S S E S I N R O D E L E M E N T S ( C R O D ) ELEMENT AXIAL SAFETY TORSIONAL SAFETY ELEMENT AXIAL SAFETY TORSIONAL SAFETY ID. STRESS MARGIN STRESS MARGIN ID. STRESS MARGIN STRESS MARGIN E E E E E E E E
43 WORKSHOP 2 Simply-Supported Truss 24. MSC/NASTRAN Users have finished this exercise. MSC/PATRAN Users should proceed to the next step. 25. Proceed with the Reverse Translation process, that is, importing the prob2.op2 results file into MSC/PATRAN. To do this, return to the Analysis form and proceed as follows: Analysis Action: Read Output 2 Object: Result Entities Method: Translate Select Results File... Filter Available Files: prob2.op2 26. When the translation is complete and the Heartbeat turns green, bring up the Results form. Results Action: Create Object: Fringe Select Results Case(s): Select Fringe Result: Quantity: temperature_load, Static Subcase Displacements, Translational Magnitude MSC/NASTRAN 101 Exercise Workbook 2-43
44 To change the target entites of the plot, click on the Target Entities icon. Target Entites Target Entity: Select Materials: Materials southern_pine steel To change the display attributes of the plot, click on the Display Attributes icon. Display Attributes Style: Discrete/Smooth To change the plot options, click on the Plot Options icon. Plot Options Coordinate Transformation: None 26a. Next, add the deformation options to the plot. Results Action: Create Object: Deformation 2-44 MSC/NASTRAN 101 Exercise Workbook
45 WORKSHOP 2 Simply-Supported Truss To change the target entites of the plot, click on the Target Entites icon. Target Entities Target Entity: Select Materials: Materials southern_pine steel To change the properties of the plot, click on the Display Attributes icon. Display Attributes Show Undeformed Line Style: If you wish to reset your display graphics to the state it was in before you began post-processing your model, remember to select the Reset Graphics icon. Reset Graphics You can go back and select any Results Case, Fringe Results or Deformation Results you are interested in. Quit MSC/PATRAN when you have completed this exercise. MSC/NASTRAN 101 Exercise Workbook 2-45
46 2-46 MSC/NASTRAN 101 Exercise Workbook
Linear Static Analysis of a Simply-Supported Truss
LESSON 8 Linear Static Analysis of a Simply-Supported Truss Objectives: Create a finite element model by explicitly defining node locations and element connectivities. Define a MSC/NASTRAN analysis model
More informationRigid Element Analysis with RBE2 and CONM2
WORKSHOP PROBLEM 5 Rigid Element Analysis with RBE2 and CONM2 Y Y Z Z X Objectives: Idealize a rigid end using RBE2 elements. Define a concentrated mass, to represent the weight of the rigid enclosure
More informationElastic Stability of a Plate
WORKSHOP PROBLEM 7 Elastic Stability of a Plate Objectives Produce a Nastran input file. Submit the file for analysis in MSC/NASTRAN. Find the first five natural modes of the plate. MSC/NASTRAN 101 Exercise
More informationModal Analysis of A Flat Plate using Static Reduction
WORKSHOP PROBLEM 2 Modal Analysis of A Flat Plate using Static Reduction Objectives Reduce the dynamic math model, created in Workshop 1, to one with fewer degrees of freedom. Produce a MSC/NASTRAN input
More informationRigid Element Analysis with RBAR
WORKSHOP 4 Rigid Element Analysis with RBAR Y Objectives: Idealize the tube with QUAD4 elements. Use RBAR elements to model a rigid end. Produce a Nastran input file that represents the cylinder. Submit
More informationModal Analysis of a Beam (SI Units)
APPENDIX 1a Modal Analysis of a Beam (SI Units) Objectives Perform normal modes analysis of a cantilever beam. Submit the file for analysis in MSC.Nastran. Find the first three natural frequencies and
More informationElasto-Plastic Deformation of a Thin Plate
WORKSHOP PROBLEM 6 Elasto-Plastic Deformation of a Thin Plate W P y L x P Objectives: Demonstrate the use of elasto-plastic material properties. Create an accurate deformation plot of the model. Create
More informationNonlinear Creep Analysis
WORKSHOP PROBLEM 7 Nonlinear Creep Analysis Objectives: Demonstrate the use of creep material properties. Examine the strain for each subcase. Create an XY plot of Load vs. Displacement for all the subcases.
More informationLinear Static Analysis of a Spring Element (CELAS)
Linear Static Analysis of a Spring Element (CELAS) Objectives: Modify nodal analysis and nodal definition coordinate systems to reference a local coordinate system. Define bar elements connected with a
More informationElasto-Plastic Deformation of a Truss Structure
WORKSHOP PROBLEM 8 Elasto-Plastic Deformation of a Truss Structure Objectives: Demonstrate the use of elasto-plastic material properties. Create an enforced displacement on the model. Create an XY plot
More informationLoad Analysis of a Beam (using a point force and moment)
WORKSHOP 13a Load Analysis of a Beam (using a point force and moment) 100 lbs Y Z X Objectives: Construct a 1d representation of a beam. Account for induced moments from an off-center compressive load
More informationModal Analysis of a Flat Plate
WORKSHOP 1 Modal Analysis of a Flat Plate Objectives Produce a MSC.Nastran input file. Submit the file for analysis in MSC.Nastran. Find the first five natural frequencies and mode shapes of the flat plate.
More informationLinear Buckling Load Analysis (without spring)
WORKSHOP PROBLEM 4a Linear Buckling Load Analysis (without spring) Objectives: Demonstrate the use of linear buckling analysis. MSC/NASTRAN 103 Exercise Workbook 4a-1 4a-2 MSC/NASTRAN 103 Exercise Workbook
More informationDirect Transient Response Analysis
WORKSHOP PROBLEM 3 Direct Transient Response Analysis Objectives Define time-varying excitation. Produce a MSC/NASTRAN input file from dynamic math model created in Workshop 1. Submit the file for analysis
More informationWORKSHOP 33 A1 A2 A1. Subcase 1 4 Subcase 2 X: -16,000 lbs. X: 16,000 lbs Y: -12,000 lbs. Y: -12,000 lbs. Objectives:
WORKSHOP 33 y 2 x 1 3 A1 A2 A1 1 2 3 Subcase 1 4 Subcase 2 X: -16,000 lbs X: 16,000 lbs Y: -12,000 lbs Y: -12,000 lbs Objectives: Optimize the following three-bar truss problem subject to static loading.
More informationModal Transient Response Analysis
WORKSHOP PROBLEM 4 Modal Transient Response Analysis Z Y X Objectives Define time-varying excitation. Produce a MSC/NASTRAN input file from a dynamic math model, created in Workshop 1. Submit the file
More informationModal Transient Response Analysis
WORKSHOP 22 Modal Transient Response Analysis Z Y X Objectives Define time-varying excitation. Produce a MSC.Nastran input file from a dynamic math model, created in Workshop 1. Submit the file for analysis
More informationDirect Transient Response Analysis
WORKSHOP 3 Direct Transient Response Analysis Objectives Define time-varying excitation. Produce a MSC.Nastran input file from dynamic math model created in Workshop 1. Submit the file for analysis in
More informationShear and Moment Reactions - Linear Static Analysis with RBE3
WORKSHOP 10a Shear and Moment Reactions - Linear Static Analysis with RBE3 250 10 15 M16x2 bolts F = 16 kn C B O 60 60 200 D A Objectives: 75 75 50 300 Create a geometric representation of the bolts. Use
More informationNormal Modes - Rigid Element Analysis with RBE2 and CONM2
APPENDIX A Normal Modes - Rigid Element Analysis with RBE2 and CONM2 T 1 Z R Y Z X Objectives: Create a geometric representation of a tube. Use the geometry model to define an analysis model comprised
More informationModal Transient Response Analysis
WORKSHOP 4 Modal Transient Response Analysis Z Y X Objectives Define time-varying excitation. Produce a MSC.Nastran input file from a dynamic math model, created in Workshop 1. Submit the file for analysis
More informationNormal Modes - Rigid Element Analysis with RBE2 and CONM2
APPENDIX A Normal Modes - Rigid Element Analysis with RBE2 and CONM2 T 1 Z R Y Z X Objectives: Create a geometric representation of a tube. Use the geometry model to define an analysis model comprised
More informationNormal Modes - Rigid Element Analysis with RBE2 and CONM2
LESSON 16 Normal Modes - Rigid Element Analysis with RBE2 and CONM2 Y Y Z Z X Objectives: Create a geometric representation of a tube. Use the geometry model to define an analysis model comprised of plate
More informationRestarting a Linear Static Analysis of a Simply- Supported Stiffened Plate
WORKSHOP 15 Restarting a Linear Static Analysis of a Simply- Supported Stiffened Plate Objectives: Submit a job to MSC.Nastran for analysis and save the restart files. (SCR = NO) Perform a restart on a
More informationAPPENDIX B. PBEAML Exercise. MSC.Nastran 105 Exercise Workbook B-1
APPENDIX B PBEAML Exercise MSC.Nastran 105 Exercise Workbook B-1 B-2 MSC.Nastran 105 Exercise Workbook APPENDIX B PBEAML Exercise Exercise Procedure: 1. Create a new database called pbeam.db. File/New...
More informationNormal Modes with Differential Stiffness
WORKSHOP PROBLEM 14b Normal Modes with Differential Stiffness Objectives Analyze a stiffened beam for normal modes. Produce an MSC/ NASTRAN input file that represent beam and load. Submit for analysis.
More informationModal Analysis of Interpolation Constraint Elements and Concentrated Mass
APPENDIX B Modal Analysis of Interpolation Constraint Elements and Concentrated Mass Y Y Z Z X Objectives: Utilize the analysis model created in a previous exercise. Run an MSC.Nastran modal analysis with
More informationSpring Element with Nonlinear Analysis Parameters (Multi-Step Analysis)
WORKSHOP 32c Spring Element with Nonlinear Analysis Parameters (Multi-Step Analysis) Objectives: Demonstrate the effects of geometric nonlinear analysis in SOL 106 (nonlinear statics). incremental loads
More informationThe Essence of Result Post- Processing
APPENDIX E The Essence of Result Post- Processing Objectives: Manually create the geometry for the tension coupon using the given dimensions then apply finite elements. Manually define material and element
More informationAlternate Bar Orientations
APPENDIX N Alternate Bar Orientations Objectives: The effects of alternate bar orientation vector. MSC.Nastran 120 Exercise Workbook N-1 N-2 MSC.Nastran 120 Exercise Workbook APPENDIX N Alternate Bar Orientations
More informationLarge-Scale Deformation of a Hyperelastic Material
WORKSHOP PROBLEM 5 Large-Scale Deformation of a Hyperelastic Material Objectives: Demonstrate the use of hyperelastic material properties. Create an accurate deformation plot of the model. MSC/NASTRAN
More informationNormal Modes Analysis of a Simply-Supported Stiffened Plate
APPENDIX C Normal Modes Analysis of a Simply-Supported Stiffened Plate Objectives: Manually convert a Linear Static analysis (Sol 101) input file to a Normal Modes analysis (Sol 103) input file. Learn
More informationSpring Element with Nonlinear Analysis Parameters (filter using restart)
WORKSHOP PROBLEM 1e Spring Element with Nonlinear Analysis Parameters (filter using restart) Objectives: Demonstrate another use of the restart feature in a multistep analysis by keeping only the first
More informationMaterials, Load Cases and LBC Assignment
LESSON 4 Materials, Load Cases and LBC Assignment 5.013 5.000 4.714 30000 4.429 4.143 3.858 3.572 3.287 3.001 2.716 2.430 2.145 1.859 20000 1.574 1.288 default_fringe : 1.003 Max 2.277 @Elm 40079.1 Min
More informationMulti-Step Analysis of a Cantilever Beam
LESSON 4 Multi-Step Analysis of a Cantilever Beam LEGEND 75000. 50000. 25000. 0. -25000. -50000. -75000. 0. 3.50 7.00 10.5 14.0 17.5 21.0 Objectives: Demonstrate multi-step analysis set up in MSC/Advanced_FEA.
More informationIntroduction to MSC.Patran
Exercise 1 Introduction to MSC.Patran Objectives: Create geometry for a Beam. Add Loads and Boundary Conditions. Review analysis results. MSC.Patran 301 Exercise Workbook - Release 9.0 1-1 1-2 MSC.Patran
More informationStiffened Plate With Pressure Loading
Supplementary Exercise - 3 Stiffened Plate With Pressure Loading Objective: geometry and 1/4 symmetry finite element model. beam elements using shell element edges. MSC.Patran 301 Exercise Workbook Supp3-1
More informationFinite Element Analysis Using NEi Nastran
Appendix B Finite Element Analysis Using NEi Nastran B.1 INTRODUCTION NEi Nastran is engineering analysis and simulation software developed by Noran Engineering, Inc. NEi Nastran is a general purpose finite
More informationTransient Response of a Rocket
Transient Response of a Rocket 100 Force 0 1.0 1.001 3.0 Time Objectives: Develope a finite element model that represents an axial force (thrust) applied to a rocket over time. Perform a linear transient
More informationLinear Bifurcation Buckling Analysis of Thin Plate
LESSON 13a Linear Bifurcation Buckling Analysis of Thin Plate Objectives: Construct a quarter model of a simply supported plate. Place an edge load on the plate. Run an Advanced FEA bifurcation buckling
More informationSliding Block LESSON 26. Objectives: Demonstrate the use of Contact LBCs in a simple exercise.
LESSON 26 Sliding Block 5 Objectives: Demonstrate the use of Contact LBCs in a simple exercise. Present method for monitoring a non-linear analysis progress. 26-1 26-2 LESSON 26 Sliding Block Model Description:
More informationPost-Buckling Analysis of a Thin Plate
LESSON 13b Post-Buckling Analysis of a Thin Plate Objectives: Construct a thin plate (with slight imperfection) Place an axial load on the plate. Run an Advanced FEA nonlinear static analysis in order
More informationModeling a Shell to a Solid Element Transition
LESSON 9 Modeling a Shell to a Solid Element Transition Objectives: Use MPCs to replicate a Solid with a Surface. Compare stress results of the Solid and Surface 9-1 9-2 LESSON 9 Modeling a Shell to a
More informationHelical Spring. Supplementary Exercise - 6. Objective: Develop model of a helical spring
Supplementary Exercise - 6 Helical Spring Objective: Develop model of a helical spring Perform a linear analysis to obtain displacements and stresses. MSC.Patran 301 Exercise Workbook Supp6-1 Supp6-2 MSC.Patran
More informationEngine Gasket Model Instructions
SOL 600 Engine Gasket Model Instructions Demonstrated:! Set up the Model Database! 3D Model Import from a MSC.Nastran BDF! Creation of Groups from Element Properties! Complete the Material Models! Import
More informationLinear and Nonlinear Analysis of a Cantilever Beam
LESSON 1 Linear and Nonlinear Analysis of a Cantilever Beam P L Objectives: Create a beam database to be used for the specified subsequent exercises. Compare small vs. large displacement analysis. Linear
More informationHeat Transfer Analysis of a Pipe
LESSON 25 Heat Transfer Analysis of a Pipe 3 Fluid 800 Ambient Temperture Temperture, C 800 500 2 Dia Fluid Ambient 10 20 30 40 Time, s Objectives: Transient Heat Transfer Analysis Model Convection, Conduction
More informationLinear Static Analysis of a Simply-Supported Stiffened Plate
WORKSHOP 7 Linear Static Analysis of a Simply-Supported Stiffened Plate Objectives: Create a geometric representation of a stiffened plate. Use the geometry model to define an analysis model comprised
More informationFigure E3-1 A plane struss structure under applied loading. Start MARC Designer. From the main menu, select STATIC STRESS ANALYSIS.
Example 3 Static Stress Analysis on a Plane Truss Structure Problem Statement: In this exercise, you will use MARC Designer software to carry out a static stress analysis on a simple plane truss structure,
More informationGeometric Linear Analysis of a Cantilever Beam
WORKSHOP PROBLEM 2a Geometric Linear Analysis of a Cantilever Beam Objectives: Demonstrate the use of geometric linear analysis. Observe the behavior of the cantilever beam under four increasing load magnitudes.
More informationUsing Groups and Lists
LESSON 15 Using Groups and Lists Objectives: Build a finite element model that includes element properties and boundary conditions. Use lists to identify parts of the model with specified attributes. Explore
More informationImporting a PATRAN 2.5 Model into P3
LESSON 1 Importing a PATRAN 2.5 Model into P3 Objectives: Read a PATRAN 2.5 neutral file into P3. Import PATRAN 2.5 result files into your P3 database. Work with multiple load cases. PATRAN 303 Exercise
More informationBackground CE 342. Why RISA-2D? Availability
Background CE 342 RISA-2D RISA-2D is a structural analysis program, which can model: Beams, frames, trusses and plates. Any linear elastic structural material. Typical supports, such as pins, rollers and
More informationSpatial Variation of Physical Properties
LESSON 5 Spatial Variation of Physical Properties Aluminum Steel 45 Radius 1 Radius 3 Radius 4 Objective: To model the variation of physical properties as a function of spatial coordinates. MSC/NASTRAN
More informationElasto-Plastic Deformation of a Truss Structure
WORKSHOP PROBLEM 8 Elasto-Plastic Deformation of a Truss Structure Objectives: Demonstrate the use of elastic-plastic material properties. Create an enforced displacement on the model. Run an MSC/NASTRAN
More informationFINITE ELEMENT ANALYSIS OF A PLANAR TRUSS
FINITE ELEMENT ANALYSIS OF A PLANAR TRUSS Instructor: Professor James Sherwood Revised: Michael Schraiber, Dimitri Soteropoulos, Sanjay Nainani Programs Utilized: HyperMesh Desktop v2017.2, OptiStruct,
More informationLoad Lug Model EXERCISE 6. Objective: Write a function to apply the loads and element properties to the finite element mesh of the lug.
EXERCISE 6 Load Lug Model Objective: Write a function to apply the loads and element properties to the finite element mesh of the lug. PATRAN 304 Exercise Workbook 6-1 6-2 PATRAN 304 Exercise Workbook
More informationPost Processing of Displacement Results
WORKSHOP 16 Post Processing of Displacement Results Objectives: Examine the deformation of the MSC.Nastran model to evaluate the validity of the assumptions made in the creation of the mesh density and
More informationSpatial Variation of Physical Properties
LESSON 13 Spatial Variation of Physical Properties Aluminum Steel 45 Radius 1 Radius 3 Radius 4 Objective: To model the variation of physical properties as a function of spatial coordinates. PATRAN301ExericseWorkbook-Release7.5
More informationFINITE ELEMENT ANALYSIS OF A PLANAR TRUSS
FINITE ELEMENT ANALYSIS OF A PLANAR TRUSS Instructor: Professor James Sherwood Revised: Michael Schraiber, Dimitri Soteropoulos Programs Utilized: HyperMesh Desktop v12.0, OptiStruct, HyperView This tutorial
More informationPost-Processing Modal Results of a Space Satellite
LESSON 8 Post-Processing Modal Results of a Space Satellite 30000 7.61+00 5.39+00 30002 30001 mode 1 : Max 5.39+00 @Nd 977 Objectives: Post-process model results from an DB file. View and animate the eigenvector
More informationMSC/PATRAN LAMINATE MODELER COURSE PAT 325 Workbook
MSC/PATRAN LAMINATE MODELER COURSE PAT 325 Workbook P3*V8.0*Z*Z*Z*SM-PAT325-WBK - 1 - - 2 - Table of Contents Page 1 Composite Model of Loaded Flat Plate 2 Failure Criteria for Flat Plate 3 Making Plies
More informationShell-to-Solid Element Connector(RSSCON)
WORKSHOP 11 Shell-to-Solid Element Connector(RSSCON) Solid Shell MSC.Nastran 105 Exercise Workbook 11-1 11-2 MSC.Nastran 105 Exercise Workbook WORKSHOP 11 Shell-to-Solid Element Connector The introduction
More informationSliding Split Tube Telescope
LESSON 15 Sliding Split Tube Telescope Objectives: Shell-to-shell contact -accounting for shell thickness. Creating boundary conditions and loads by way of rigid surfaces. Simulate large displacements,
More informationMass Properties Calculations
LESSON 15 Mass Properties Calculations Objectives Import a unigraphics express file and apply mass properties to the propeller. PAT302 Exercise Workbook MSC/PATRAN Version 8.0 15-1 15-2 PAT302 Exercise
More informationPost-Processing Static Results of a Space Satellite
LESSON 7 Post-Processing Static Results of a Space Satellite 3.84+05 3.58+05 3.33+05 3.07+05 2.82+05 3.84+05 2.56+05 2.30+05 2.05+05 1.79+05 1.54+05 1.28+05 1.02+05 7.68+04 0. 5.12+04 Z Y X Objectives:
More informationAnalysis Steps 1. Start Abaqus and choose to create a new model database
Source: Online tutorials for ABAQUS Problem Description The two dimensional bridge structure, which consists of steel T sections (b=0.25, h=0.25, I=0.125, t f =t w =0.05), is simply supported at its lower
More informationSpring Element with Nonlinear Analysis Parameters (large displacements off)
WORKSHOP PROBLEM 1a Spring Element with Nonlinear Analysis Parameters (large displacements off) Objectives: Create a model of a simple rod and grounded spring system. Apply the appropriate constraints
More informationTutorial 1: Welded Frame - Problem Description
Tutorial 1: Welded Frame - Problem Description Introduction In this first tutorial, we will analyse a simple frame: firstly as a welded frame, and secondly as a pin jointed truss. In each case, we will
More informationImporting Results using a Results Template
LESSON 15 Importing Results using a Results Template Objectives: Write a custom nodal and displacement results template. Import a Patran 2.5 Neutral File model. Import a Patran 2.5 Results File. Perform
More informationCylinder with T-Beam Stiffeners
LESSON 17 Cylinder with T-Beam Stiffeners X Y Objectives: Create a cylinder and apply loads. Use the beam library to add stiffeners to the cylinder. PATRAN 302 Exercise Workbook - Release 8.0 17-1 17-2
More informationCME-TRUSS (Version 2.1) User's Manual
CME-TRUSS (Version 2.1) User's Manual INTRODUCTION CME-TRUSS is an interactive program for structural analysis of two-dimensional trusses. The software is written in the Microsoft Visual Basic for Windows
More informationNonlinear Creep Analysis
WORKSHOP PROBLEM 7 Nonlinear Creep Analysis Objectives: Create the appropriate load cases for nonlinear static and nonlinear creep loads. Examine the strain for each subcase. Run an MSC/NASTRAN nonlinear
More informationThermal Analysis Using MSC.Nastran
MSC.Software Corporation 815 Colorado Boulevard Los Angeles, California 90041-1777 Tel: (323) 258-9111 Fax: (323) 259-3838 United States MSC.Patran Support Tel: 1-800-732-7284 Fax: 714-9792990 Tokyo, Japan
More informationSpring Element with Nonlinear Analysis Parameters (Multi-step Analysis)
WORKSHOP PROBLEM 1c Spring Element with Nonlinear Analysis Parameters (Multi-step Analysis) Objectives: Import the model from the previous exercise. Apply incremental load through multiple subcases. Submit
More informationMULTI-SPRING REPRESENTATION OF FASTENERS FOR MSC/NASTRAN MODELING
MULTI-SPRING REPRESENTATION OF FASTENERS FOR MSC/NASTRAN MODELING Alexander Rutman, Ph. D, Joseph Bales-Kogan, M. Sc. ** Boeing Commercial Airplane Group Strut Structures Technology MS K95-04 380 South
More informationLearning Module 8 Shape Optimization
Learning Module 8 Shape Optimization What is a Learning Module? Title Page Guide A Learning Module (LM) is a structured, concise, and self-sufficient learning resource. An LM provides the learner with
More information2: Static analysis of a plate
2: Static analysis of a plate Topics covered Project description Using SolidWorks Simulation interface Linear static analysis with solid elements Finding reaction forces Controlling discretization errors
More informationLinear Static Analysis for a 3-D Slideline Contact
WORKSHOP PROBLEM 10a Linear Static Analysis for a 3-D Slideline Contact Objectives: Demonstrate the use of slideline contact. Run an MSC/NASTRAN linear static analysis. Create an accurate deformation plot
More informationLinear Buckling Load Analysis (without spring)
WORKSHOP PROBLEM 4a Linear Buckling Load Analysis (without spring) Objectives: Create and prepare the appropriate model for the analysis. Demonstrate the use of linear buckling analysis. MSC/NASTRAN for
More informationModal Analysis of A Flat Plate using Static Reduction
WORKSHOP PROBLEM 2 Modal Analysis of A Flat Plate using Static Reduction Objectives Reduce the dynamic math model, created in Workshop 1, to one with fewer degrees of freedom. Apply the static reduction
More informationRigid Element Analysis with RBE2 and CONM2
WORKSHOP 8 Rigid Element Analysis with RBE2 and CONM2 Y Z X Objectives: Create a geometric representation of a tube. Use the geometry model to define an analysis model comprised of plate elements. Idealize
More informationMSC.Patran s Freebody Tool. Isaac Newton s First and Favorite
MSC.Patran s Freebody Tool Isaac Newton s First and Favorite Created: 6/15/2005 Updated: 10/22/2007 What is a Freebody? V M Freebody Tool Designed to provide an intuitive interface to MSC.Nastran s Grid
More information= Set the units Click on the units icon, and change the default units to lbs and inches for:
CE 331, Fall 2012 Guide for Using RISA3D to Model a Balsa Structure 1 / 9 Example Bridge. An example structure is shown below. Typical results for the RISA model of this structure are shown throughout
More informationAnsys Lab Frame Analysis
Ansys Lab Frame Analysis Analyze the highway overpass frame shown in Figure. The main horizontal beam is W24x162 (area = 47.7 in 2, moment of inertia = 5170 in 4, height = 25 in). The inclined members
More information= 21
CE 331, Spring 2011 Guide for Using RISA3D to Model a Balsa Structure 1 / 9 0. Example Bridge. An example structure is shown below. Typical results for the RISA model of this structure are shown throughout
More informationComparison of Two Heat Sink Designs
Exercise 6 Comparison of Two Heat Sink Designs Objective: Model two competing finned heat sinks. These will be 2D axisymmetric slices. PATRAN 312 Exercises -Version 7.5 6-1 6-2 PATRAN 312 Exercises - Version
More informationStatic and Normal Mode Analysis of a Space Satellite
LESSON 6 Static and Normal Mode of a Space Satellite Z Y X Objectives: Setup and analyze the satellite model for a normal modes and static analysis.. Learn to modify the default subcase parameters, solution
More informationEXAMPLE 1. Static Analysis of Cantilever Column (Fixed-Base Column)
EXAMPLE 1 Static Analysis of Cantilever Column (Fixed-Base Column) Calculate the top displacement, axial force, shear force and bending moment diagrams for the fixed base column described in the figure
More informationFINITE ELEMENT ANALYSIS OF A PLANAR TRUSS
Problem Description: FINITE ELEMENT ANALYSIS OF A PLANAR TRUSS Instructor: Professor James Sherwood Revised: Dimitri Soteropoulos Programs Utilized: Abaqus/CAE 6.11-2 This tutorial explains how to build
More informationDirect Transient Response with Base Excitation
WORKSHOP PROBLEM 7 Direct Transient Response with Base Excitation Z Y X Objectives Create a geometric representation of a flat rectangular plate. Use the geometry model to define an analysis model comprised
More informationME 442. Marc/Mentat-2011 Tutorial-1
ME 442 Overview Marc/Mentat-2011 Tutorial-1 The purpose of this tutorial is to introduce the new user to the MSC/MARC/MENTAT finite element program. It should take about one hour to complete. The MARC/MENTAT
More informationMerging Databases LESSON 2. Objectives: Construct two databases which have distinct similarities and differences.
LESSON 2 Merging Databases Objectives: Construct two databases which have distinct similarities and differences. See how PATRAN resolves model conflicts and differences when the two databases are imported
More informationME Optimization of a Truss
ME 475 - Optimization of a Truss Analysis Problem Statement: The following problem will be analyzed using Abaqus and optimized using HEEDS. 4 5 8 2 11 3 10 6 9 1 7 12 6 m 300 kn 300 kn 22 m 35 m Figure
More information3. Check by Eurocode 3 a Steel Truss
TF 3. Check by Eurocode 3 a Steel Truss Applicable CivilFEM Product: All CivilFEM Products Level of Difficulty: Moderate Interactive Time Required: 40 minutes Discipline: Structural Steel Analysis Type:
More informationLesson 6: Assembly Structural Analysis
Lesson 6: Assembly Structural Analysis In this lesson you will learn different approaches to analyze the assembly using assembly analysis connection properties between assembly components. In addition
More informationVerification and Property Assignment
LESSON 9 Verification and Property Assignment Objectives: Prepare the model for analysis by eliminating duplicate nodes and verifying element attributes. material and element properties. PATRAN 301 Exercise
More informationME Optimization of a Frame
ME 475 - Optimization of a Frame Analysis Problem Statement: The following problem will be analyzed using Abaqus. 4 7 7 5,000 N 5,000 N 0,000 N 6 6 4 3 5 5 4 4 3 3 Figure. Full frame geometry and loading
More informationTemperature Dependent Material Properties
WORKSHOP 8 Temperature Dependent Material Properties Objective: You will create a 2D material slice consisting of two materials with temperature dependent material properties. You will visually and qualitatively
More informationTorsional-lateral buckling large displacement analysis with a simple beam using Abaqus 6.10
Torsional-lateral buckling large displacement analysis with a simple beam using Abaqus 6.10 This document contains an Abaqus tutorial for performing a buckling analysis using the finite element program
More information